Stuck? 
support@mecway.com
support@mecway.com
Mecway
FEA
modelling of epoxy
Hi Guys
I hope that everyone is well. This is not a Mecway query, but more of a general FEA query (note that I am a Mecway user and owner of a license)
Has anyone worked with the modelling of epoxy in an FEA environment?
Please refer to the attached image for a simplification of my scenario.
Assuming that I have all the mechanical properties for the epoxy and keeping in mind that its thickness is going to be extremely small.
The most logical way to model is to use plate elements for all steel work and model the epoxy as brick elements. The mesh of the contacted surfaces will need to share nodes to reduce solving time. The problem comes in with the thickness of the brick elements, the mesh over the thickness will be extremely poor thus producing poor results.
The other option is to model a reasonably thick arrangement of brick elements and change the stiffness (K = EA/I) so that it acts as it should. This however will require correlation to actual testing which is unfeasible.
The last option I thought of is to use contact between the surfaces based on the properties of the epoxy. This however will not allow for shear transfer.
Has anyone got any suggestions as to how this can be performed?
I hope that everyone is well. This is not a Mecway query, but more of a general FEA query (note that I am a Mecway user and owner of a license)
Has anyone worked with the modelling of epoxy in an FEA environment?
Please refer to the attached image for a simplification of my scenario.
Assuming that I have all the mechanical properties for the epoxy and keeping in mind that its thickness is going to be extremely small.
The most logical way to model is to use plate elements for all steel work and model the epoxy as brick elements. The mesh of the contacted surfaces will need to share nodes to reduce solving time. The problem comes in with the thickness of the brick elements, the mesh over the thickness will be extremely poor thus producing poor results.
The other option is to model a reasonably thick arrangement of brick elements and change the stiffness (K = EA/I) so that it acts as it should. This however will require correlation to actual testing which is unfeasible.
The last option I thought of is to use contact between the surfaces based on the properties of the epoxy. This however will not allow for shear transfer.
Has anyone got any suggestions as to how this can be performed?
Howdy, Stranger!
It looks like you're new here. If you want to get involved, click one of these buttons!
Comments
I have no idea if this would be later useful to you and how accurate would be the results but ¿have you consider to model with the set Plate/Epoxy/Beam Plate as a unique “laminate shell” where each layer has its own properties. There is Shear modulus involved between layers so you can sustain shear stress between laminates.
For Example:
15 mm , 0º, 210 MPa, 210,…….
.2 mm , 0º, 43 MPa, 43,…….
15 mm , 0º, 210 MPa, 210,…….
Maybe someone with more experience on laminates can comment about accuracy problems of this strategy.
I’m curious about your problem.
¿Are you dealing with finding tighten force required to avoid slipping plates that have been painted with some epoxy cover?
Regards
yes as disla said, i would try the laminate feature and the ccx solver. i have used that and it works good. you can also use a composite shell model, if you have bulk material properties for the laminate. using the laminate feature is generally easier because you don't have to figure out the bulk material properties for the laminate. it also allows you to experiment with laminate orientation and number of lams. i don't know that you are doing a traditional composite analysis here. however, what you describe seems like it could be done using one of these two features. if you want an example file to learn from, I can post one of the test models I did awhile ago. It did take me quite a long time to figure out how to model composites.
But, flat hex20 solids are pretty good with high aspect ratios. You may only need one or two layers of solid elements using them.
I now realize that laminates could be an easy way to gain accuracy in a computation modeled with shell elements.
I mean, ccx expands shells into solids. Defining the shell as a laminate with all its sheets with the same properties we could provide the desirable number of elements per thickness recommended in general solid modeling without effort.
It could be an easy way to convert a shell model into a solid model in ccx without touching more than the material properties. ¿Am I losing something?
What I would suggest now I see the problem more in detail would be to keep one plate as pure steel and the other as laminate with Epoxy and Steel components. This way you could provide more mesh refinement only in the laminate side and allow for both sides to move independently in case you want to introduce some more details in the bolted area behaviour.
on the material property input for laminates you enter the thickness. so i'm not sure you have to do what you were thinking. as far as the aspect ratios, it doesn't seem to matter. i don't understand why that is. however, based on the results, i'm not seeing any ill affects from the thin solids. both quads and tets get expanded making very thin solids. you have control over what gets created via the inputs. so it's a lot simpler than you are thinking. you can set it up in a way that gives a good aspect ratio sometimes.
lastly, mecway offers an offset option which you may have to use depending on the geometry. it depends on any radius or bends that your model may have. when the solids get expanded it can cause them to intersect and the solve to fail. so then you would expand the model in the other direction. this part is trial and error. i don't know of a clear way to know if there is going to be an intersection issue or not. this affects how you create the cad model though. so it creates a lot of work if you pick one direction and it doesn't work out. fortunately, there are only three choices. midplane, expand inward, or expand outwards. sometimes i make all three models in cad, since i don't know which ones will work.
one oddity though is that when the elements get expanded they are no longer touching in places with a radius or bend. i'm assuming that they were actually connected for the solve and not touching is just a graphical thing you have to live with.
i attached a picture of the material property inputs.
Edited
You can use this test model to see how the lam properties work. For the case of steel, epoxy, steel; it would be easy to modify the properties for that.
The model shape was to try and trigger this issue that forces you to expand the model in one direction or the other. I didn't trigger it here though. It has to do with the radius and the thickness. Not sure what the magical factors are. But if you run into that issue you can use shell offset.
Edit; I should add that when I had the issue of needing to use shell offset, all my bends where in the same direction. This model purposely had bends in both directions. So using the midplane should be the only option. So if you had the issue it would most likely mean the model was too thick for the radius used and you wouldn't have any option but to make it thinner or change the radius values. The offset fix wouldn't work if you had tight bends in opposite directions.
The first of all, congratulations for your nice example posted.
I was wondering if you have extra information or theory about your "vibratory_allowable_stress_MPa_for_XXX" formula embedded in your liml file?
Thank you in advance
MANUEL MARTÍN.
thanks. i have more example files. i tried to build a library of materials from info i found online. the main thing of importance for me is fatigue strength. the formulas i added make it easy for me to see the steady stress in percent of max and then the fatigue strength. i use to have to do it the old way in a spreadsheet with a soderberg diagram. the mecway formulas are really awesome and i tried to take advantage of them. you can now see the vibratory allowable on the whole model. no need to go back to the spreadsheet anymore. however, the formula is the soderberg diagram formula based on the listed fatigue strength and yield strength. so that formula/method is conservative. but that's good in my case. the properties are all just examples based on internet info. for real engineering you have to do a lot of material and part testing. i'm retired and just do this for fun. if you want i can put together my examples, library, and reference info that i saved. i don't think i saved all the reference info but i have most of it. since it's from the internet, it may not be that accurate. i started adding materials based on forum help i provided. so some of the materials i never worked with. spring steel and ryton come to mind there. the composites is something i wanted to have and searched a lot to find the best info i could. however, it's really limited. i started with a coupon method that you can use with shell models. i eventually went to the laminate method that works off of general composite and epoxy properties. i've been happy with that method but it's a bit more compute intensive. the coupon method requires specific layup testing. i only found one material online with the necessary data. however, some of the data was missing and the fatigue testing wasn't standard for aerospace. so the coupon data isn't really right. you would have to do all the testing to go that way. i think the laminate properties are fine and that method works well. sometimes it can take awhile to solve due to all the extra elements. however, you get much more resolution through the thickness which is really nice.
anthony
I have made some simple test and readings to understand Victor's sentence
"You may still get an improvement due to more integration points though".
Using many layers of the same material do not provide more accuracy. In fact, it seems to be worse than a simple shell element when there are less than three layers.
Looking at the ccx report , laminates are using a maximum of 8 integration points per layer while shell has 27.
By other hand , if i did understand it properly, more integration points means that we can integrate the shape function more accurately to obtain the strains/stresses, but this do not mean the strain/stress is a better value (in terms of closer to reality). The laminate has the same limitations as the shell element in terms of capturing the stresses through thickness.
Now, I don’t see any reason to use laminates if there is no difference in material properties between the layers.
¿what do you guys think?
i did a lot of comparisons between solid, shell, and laminate. i didn't see much difference. however, you get more resolution through the thickness. unfortunately, there are no mesh metrics, so i'm not sure how to relate mesh quality to results. i didn't see anything horrible from any method. but you would need to compare to test data to know best. i agree though, the only real reason to use the laminate feature is if you need to, based on the material layup. some of the files i have are trivial using the same material for every lam. those are just for testing or i randomly selected a material for testing.
it would be nice if there were mesh metrics available prior to solve and if you could see which are the bad elements. ansys has those kinds of features but netgen only has some basic features. also, with the ccx shell/lam expansion, that makes it even harder for the mesh metrics. i think you would have to build the mesh prior to solve which isn't something that is happening right now. it only builds the mesh as part of the solve.
@disla, I'm surprised the difference between solids and shells is as great as shown in screenshot.9.png. I wonder if the shell's boundary conditions aren't working properly. Could you post the .liml file?
Thanks for all the comments.
The epoxy is used on a vibrating screen. I intend on taking measurements using an accelerometer at various locations and using this information to calibrate to a bolted connection and thus I can develop an empirical study of the epoxy to evaluate if it is worth it to even model the epoxy.
You are right , nodal force was not the same . More nodes, more force. My mistake .Sorry.
Example of plates under shear.
Shell left side.
Laminate with 6 layers of identical properties in the middle.
Solid on the right side
Through thickness behavior of laminate is the same as the shell element.
Good morning PROP_DESIGN:
Dear ANTHONY:
Thank you very much for your reply(on May 16th). I agree with you that “formulas” are a great tool to post-process the analysis. I always use them, especially for showing failure limits just like you.
Your formular is very interesting to know fatigue stress limits. I did some research with the file you attached. You are right, in a glimpse, you immediately know how close or far you are from failure and the number of cycles.
I think this powerful feature could be good to be improved in future versions maybe letting us some scripting instead of just a single formula..
During next week I will try to post a report about simulating cross laminated timber (in Spanish “madera laminada”) using solid elements and orthotropic materials. In my example I heavily use “formulas“ to determine the failure limit according to TSAI-WU failure criterion and limits according to EC5 and CTE-DB-M (spanish regulation about timber. It is a EC5 clon).
Regards
MANUEL